[ferrumdg]

hi,

I've been using BobCAD/CAM v25 for some time now and whilst I'm generally really pleased with it there's this one issue that's "nagging" me: Automatic Feeds & Speeds.

Whilst the notion of an integrated materials based cutting feeds and speeds calculation is really amazing - the automatically calculated values are usually way off. - FAR TOO FAST.
My CNC Mill (small 4 axis machine) has a max of 6000RPM and isn't too powerful (it's quite ok for what I need it and fits my budget quite nicely... as much as I'd like to have something like a DMG MORI, HAAS, NAKAMURA... or whatever - it'll be a while before I can afford any of that.

I currently run a trial of G-Wizzard Calculator to get a handle on the feeds/speeds and I really like it - however it requires me to double-set up my tools (inside bobcad of course and GWiz...) also I'd prefer to use the in-built option for convenience.
The speeds calculated by G-Wizzard Calc are usually "spot" on - with the few exceptions (like engraving, as this is something the low RPM of the machine really doesn't permit "nicely" but still needs to be done at times).

Now I wonder - aside from manually adjusting all feeds and speeds table within bobcat/cam (tedious to do) is there anything that can be done??

For example:

Tool: Carbide Roughing cutter, 8mm diameter, 4 flutes
Stock Material: D2 Tool Steel 1.2379, annealed.
All measurments: METRIC, feeds are in MM/MIN

Trying to do some pocketcutting - (18mm wide slot, 10mm deep 30mm long)
Standard 2 Axis Pocketing operation

Now BobCAD basically ignores whatever is going to be set for step-over, cutting depth, etc... but the calculated speeds and feeds are set to:
RPM: 4376.761
Cutting Feed Rate: 349.962
Plunge Feed Rate: 175.203
SMM: 110
Feed per Tooth: 0.020
Plunge Feed per Tooth: 0.010

Now if I'd be running the program at that neither my machine, my tools nor the material will like it...


However if I calculate the feed/speed values using G-Wizzard: (if the to not too agressive but not fully conservative (there's a slider, at 2.0))
Cut Depth: 4mm, Width: 8mm (full width (at least for the first cut) after that I'd to partial step overs of course).

RPM: 2411
Feed (mm/min): 274.5
Plunge: 68.6
SMM: 61
Chipload (mm/tooth) 0.0285

These values I can actually run with... although I'd probably slow it down a notch... but it's working.
If I set G-Wizzard on "conservative" it would generate values a good bit too slow, jfyi.


Any idea what's causing the "huge" difference to the BobCAD generated values?
Any easy way to solve this inside bobcad?

thanks!

[RAF.]

Have you tried setting up your materials cut speeds by making your own Type of Material and Cut feed Rate. I think you could probably do it here.

Milling Tools/Default/Stock Material Library

[ferrumdg]

Have you tried setting up your materials cut speeds by making your own Type of Material and Cut feed Rate. I think you could probably do it here.

Milling Tools/Default/Stock Material Library

thanks...

I'm well aware of the stock material library... but I was hoping for some way to "correct" a bunch of them without having to go through each of the needed ones manually...
I'd be spending the better part of a day matching and recalculating those I need.
Also I was wondering why BobCAM's cutting data is so off ... even the SMM suggested by material specs / most tool specs gives lower values.
Can this be some error in the conversion from inches to the metric system?

[jrmach]

Although I enter my own speeds and feeds,can you list some examples with the details of some that are way off ? There are so many factors the can alter recommended data.
I know some of the drilling on some materials are way out of line,but what else?
Personally,from experience,I usually can get close,then dial it in no problems.But with all the variables,you cannot expect an app. to be spot on.G-Wizard is good.Machinist Toolbox is what BoB uses.It is not as detailed.You can purchase the "full"app. from BoB,which gives more functionality.
Best advice I can give is use your overides to dial in,then edit program.There just no substitute for experience.Like I mentioned,just so many variables.I would just as soon all the speed/feed boxes were empty when doing cam.

[ferrumdg]

Although I enter my own speeds and feeds,can you list some examples with the details of some that are way off ? There are so many factors the can alter recommended data.
I know some of the drilling on some materials are way out of line,but what else?

I'm no longer at the shop right now (it's after 2am right now - long day)... but in my initial post I gave an example of D2 Tool Steel... that one is for example really off for most operations.

When I do the math with the spec sheets of the steel supplier and my tool data (TiAln micro-grain carbide rougher in that case)
just the suggested RPM... bobcat is somewhere around 4300 RPM - whilst otherwise I'd get 2200-2800RPMs suggested.
the SMM suggested by the steel's spec is 72... BobCAM has it at 110 (!)


It's similarly off with Titanium Grade 5, O1 Tool Steel, Aluminium (some), ...

Basically so far I don't think I had one single "success" with any material I chose with the recommended (BobCAM) feeds and speeds.
Always had to manually calculate and adjust.

I'm well aware that there are many parameters that are influencing the choice in cutting speeds... and I assume BobCAMs data is geared towards the more modern high speed machining centers with at least a CAT50 taper for tool holders and overall geared towards larger / sturdier machines.
But the offset is quite large in the data I get.

As mentioned when I use G-wizzard calculator set on a moderate level - I get near perfect feeds and speeds.
It just would be nice if I wouldn't have to buy yet another piece of software and use it parallel to bobCam just for getting the speeds right... as there's already a material database found within Bobcam...

[jrmach]

Here is the machinist toolbox data in inches.I see nothing far fetching.I will have to see what the metrics is bringing.Maybe a problem there.

[jrmach]

You could check out fs wizard.The guy who wrote the software is on PM.His name is Zero Divide.Lots of posts about it.I have a free version.Has a lot of functionality,especially suited for HSM on tougher metals.

[Ben S]

If I were in your shoes I think I would consider it worth a day to set up the material library in order to have speeds/feeds I liked from then on. In my case I only had to set up aluminum and "soft steel" so it didn't take nearly that long but it is such a pleasure to never have to make adjustments. Your situation obviously requires a bigger up-front time investment but I think it would still be worth it. Are you really spending less time now setting custom values in every part while looking for a work around?

[ferrumdg]

If I were in your shoes I think I would consider it worth a day to set up the material library in order to have speeds/feeds I liked from then on. In my case I only had to set up aluminum and "soft steel" so it didn't take nearly that long but it is such a pleasure to never have to make adjustments. Your situation obviously requires a bigger up-front time investment but I think it would still be worth it. Are you really spending less time now setting custom values in every part while looking for a work around?

Ben,

thanks ...
well No, of course you're right - I spend more time, overall to set it up time after time again.
I work with half a dozen different tool steels, two types of Titanium, a bunch of Al-alloys, some plastics, composites, wood, a bunch of non-ferrous metals...
Mostly I use full carbide tooling, some indexable carbide tooling and a small number of HSS tools (mostly reamers and two dove tail cutters).


Well I was just hoping that there's a faster work around - a way to globally influence how BobCAM interprets the values in the Stock library... or something like that...
But alas, I'll be using a software to calculate each material, at the time I'll be setting up a new job... will then store the successful values in BobCAM's stock library... and hopefully in a few month will have set all my standard materials up automatically.


Also to jrmarch:
thanks for the heads up on Zero Divides' software... I'll be giving it a try later today...



thanks to everyone for the inputs!

[jrmach]

at least on FS Wizard,if you have any questions,you can talk to the "man" that made the software.He also listens for suggestions.

[ferrumdg]

at least on FS Wizard,if you have any questions,you can talk to the "man" that made the software.He also listens for suggestions.

well that too

[Ben S]

I just downloaded the Android app. Very cool. I've been looking for something like it for a while. Thanks jrmach!

Sent from my SCH-I535 using Tapatalk

[bobcad guy]

Setting speed and feed tables is somewhat a waste of time. You can't run a full width cut the same as a perimeter pass, and a tool sticking out 1.5 from holder, isn't as rigid as a tool sticking only .75 out of holder. Yada yada

[magicniner]

Setting speed and feed tables is somewhat a waste of time. You can't run a full width cut the same as a perimeter pass, and a tool sticking out 1.5 from holder, isn't as rigid as a tool sticking only .75 out of holder. Yada yada

Surely the whole point is that if the software has some set parameters to work with it can take account of depth of cut, width of cut, climb or conventional etc. and that this is why it's worth it.
Or is this not the case?

- Nick

[jrmach]

Setting speed and feed tables is somewhat a waste of time. You can't run a full width cut the same as a perimeter pass, and a tool sticking out 1.5 from holder, isn't as rigid as a tool sticking only .75 out of holder. Yada yada

Exactly,,,,,,,,,,,Grant it,I don't know nearly all the material speeds and feeds along with figuring them out for the different unique variables,but I can figure a lot with out no table or charts.Comes from doing it for thousands of times.There is no way any tool library can take into account all things.Coatings alone,render it useless almost.Heck,holding a part in a vise compared to clamped to the table can have a big effect.It's great for getting in the ball park,especially for materials not use to running.I certainly would not count on Bob's feeds or speeds as being the "Bible",nor do I hold them responsible.Run 1st part conservatively and work your overides to optimize.Edit program accordingly,if needed.This is where the "machinist" uses his eyes and ears and experience.

Bobcad guy,I never agreed with you more,a lot of people don't agree with me on this,you get it

Even using FS Wizard,which is far Superior to Bob's,IMO,,I don't always do what they suggest,sometimes not even close.Zero Divide is a big fan of chip thinning,where as I like to hog stuff out.As there is many variables to determine feeds and speeds,there are different styles and strategies of metal removal.And that alone will also change speeds and for sure feeds.
Under powered machines,lack of rigidity,Chinese cutters,coatings,geometry of cutter,doc,loc,tool holder,coolant,dry,this goes on and on.A problem I have been running into lately is different machinability from one supplier to another for the same material,,especially 303 and 1018.How do you ever calculate that?

[zero_divide]

Jrmach,
I see you have stuck with my software since the begining or close.
You have got one of the first versions. It is more than 1 year old and a lot has changed since.
Standalone is now called HSMAdvisor.
And FSWizard (less powerful, no deflection or machine definitions) is reserved for online and mobile apps.

How about you download a latest version and spend a little time documenting things you like/dont like.
Take it through the paces, and if you decide it is the next best thing after sliced bread, i will just give you 3 seats for free?

I will need a a lot of meaningful feedback though. Dont just say "its great"!

Edit: download page is here http://hsmadvisor.com

[ferrumdg]

Setting speed and feed tables is somewhat a waste of time. You can't run a full width cut the same as a perimeter pass, and a tool sticking out 1.5 from holder, isn't as rigid as a tool sticking only .75 out of holder. Yada yada

Whilst certainly it is true, it still remains within mathematical reach to calculate at least a close-to / basic value.
And given the fact that the CAM Software actually "knows" all the cut aspects, if it's a slot, cut depth, stick-out, tool type etc... it should indeed be able to do the math.
Actually that is one of the reasons - one of them - why I guess a full-set up tool table is included in a cam package... and a materials database...?

[ferrumdg]

Exactly,,,,,,,,,,,Grant it,I don't know nearly all the material speeds and feeds along with figuring them out for the different unique variables,but I can figure a lot with out no table or charts.Comes from doing it for thousands of times.There is no way any tool library can take into account all things.Coatings alone,render it useless almost.Heck,holding a part in a vise compared to clamped to the table can have a big effect.It's great for getting in the ball park,especially for materials not use to running.I certainly would not count on Bob's feeds or speeds as being the "Bible",nor do I hold them responsible.Run 1st part conservatively and work your overides to optimize.Edit program accordingly,if needed.This is where the "machinist" uses his eyes and ears and experience.

Bobcad guy,I never agreed with you more,a lot of people don't agree with me on this,you get it

Even using FS Wizard,which is far Superior to Bob's,IMO,,I don't always do what they suggest,sometimes not even close.Zero Divide is a big fan of chip thinning,where as I like to hog stuff out.As there is many variables to determine feeds and speeds,there are different styles and strategies of metal removal.And that alone will also change speeds and for sure feeds.
Under powered machines,lack of rigidity,Chinese cutters,coatings,geometry of cutter,doc,loc,tool holder,coolant,dry,this goes on and on.A problem I have been running into lately is different machinability from one supplier to another for the same material,,especially 303 and 1018.How do you ever calculate that?

Sure, my background is with conventional machining... back then mostly with HSS Tooling... And before I've gotten into CNC almost exactly one year ago, I rarely touched Carbide Tooling (but for some indexed cutters and one or two for hard materials)... Also when I am machining manually I stand right there and if a feed is too harsh, well I've set it manually, I just crank it down.. etc... basically I find working by feedback far easier on a conventional manual machine, and experience is absolutely non-replaceable by any table or math.

However when I run more complex geometries, on work pieces I prefer not to **** up due to the plain material cost (custom forged pieces of 800 layer pattern welded steel, Titanium, ...) and use tiny cutters which cost a fortune compared to how quick they will break, I guess getting a decent starting point is a lot more important.
Also with the tiny stuff, chips if done wrong can really bog up the cut quickly.
When I was milling a series of cut outs (2.1mm wide, 3.2mm deep over all) (slotting) in Grade 6 6AL4V titanium a few backs I took the time to calculate the approx. speeds & feeds with the manufacturers and tool specs in mind - and then went on the conservative side.
I was able to do all cuts with the same tool, the tool barely showing any wear.
Where before I did the math I went through three cutters for a third of the work.... sitting down for half an hour and calculating the feeds proved to be an excellent investment.
Mind you my "guess"-work based first settings weren't *that* much off from the calculated stuff... but I guess it caused enough deflection to break the tool....

Same goes with quality cut surfaces if I want to minimize jittering etc.

[ferrumdg]

Jrmach,
I see you have stuck with my software since the begining or close.
You have got one of the first versions. It is more than 1 year old and a lot has changed since.
Standalone is now called HSMAdvisor.
And FSWizard (less powerful, no deflection or machine definitions) is reserved for online and mobile apps.

How about you download a latest version and spend a little time documenting things you like/dont like.
Take it through the paces, and if you decide it is the next best thing after sliced bread, i will just give you 3 seats for free?

I will need a a lot of meaningful feedback though. Dont just say "its great"!

Edit: download page is here HSMAdvisor : Feed And Speed Wizard For Fast Metal Removal

Zero_Divide,

Just bought HSMAdvisor yesterday and wanted to say thanks! amazing piece of software at a very reasonable price.
Pure time-saver!!
The automatic feature to paste the values into the CAM Software window is just amazing.
Also clean, purpose driven interface without too many belles and whistles ...
It's basically permanently running on the second monitor now

[jrmach]

Whilst certainly it is true, it still remains within mathematical reach to calculate at least a close-to / basic value.
And given the fact that the CAM Software actually "knows" all the cut aspects, if it's a slot, cut depth, stick-out, tool type etc... it should indeed be able to do the math.
Actually that is one of the reasons - one of them - why I guess a full-set up tool table is included in a cam package... and a materials database...?

Maybe a feature request to use a better tool library where the cam and tool library can make use of more variables and spit out more useful numbers?
Of course careful for what we wish for,,,that certainly would come at a cost $$$